The simulation was not complete and it shutdown in between. The size of tran.tran.trn is around 40 GB.

Note that I have already done this: In Analog Design Environment, Outputs -> Save All, I have checked "selected" option in "select signals to output (save)" and Outputs -> to be saved -> select on schematic and selected few nets that I wanted to save

But even after doing the above, it is still saving every net (because I'm able to plot those nets) which is the reason for such a huge tran.tran.trn file. What more should I do to stop it from saving every net? (and only save the nets that I select)

3. I can increase size of my hard disk to say 1 TB to get rid of "unable to allocate memory..." error, but my doubt is how to stop Virtuoso ADE from saving every net in the transient simulation even after doing the above mentioned steps (as in my previous post)?

5. I have tried in debian also, the problem is still there. Currently I can use cadence spectre only in debian or ubuntu.

4. I didn't understand what is the "output statement" in the netlist. So I'm pasting the netlist here. This nelist doesn't correspond to the one where I got that "Unable to allocate memory..." error. This netlist is of a different circuit generated from Virtuoso ADE after selecting the nets to be saved. I have deliberately removed some lines corresponding to circuit elements since the netlist is large.

// Generated for: spectre

// Generated on: May 31 13:01:10 2012

// Design library name: myddp

// Design cell name: divby2_vco

// Design view name: schematic

simulator lang=spectre

global 0

include "/cad/tools/cadencetools/IC5141_USR6/tools/dfII/samples/artist/ahdlLib/quantity.spectre"

include "/cad/library/UMC65/Designkits/Cadence/Models/Spectre/L65LL_V111.lib.scs" section=tt_ll_lvt12

The default in spectre is "selected", so if you uncheck everything on the "Select signals to output" line, it will be the same as explicitly picking "selected".

What "selected" does is to only save the nets marked to be saved in the outputs pane - which corresponds to the "save" statements at the bottom of the input.scs. If no nets are saved, it saves all nets (i.e. all voltages). Note it's nothing to do with what is currently selected in the schematic.

In your case, you have selected currents=nonlinear - which will end up saving a lot of data for all the currents. I'd leave device currents as blank (or selected) - that will make the data set much smaller.

As you have seen in my netlist the last but one line is "save n1" which means it should save only net n1, but I found that after the simulation is over, I'm still able to plot other nets which I didn't want it to save. To reduce size of data I would do as you said - uncheck everything in "select device currents (currents)" line. But my question is what are the settings to be done to stop ADE from being able to plot certain nets which are not selected as "saved'. It will be able to plot only if it saves it somewhere which means it occupies data.

The settings that I mentioned in the first post actually worked in my friend's system. It showed an error when trying to plot the nets which are NOT saved in the outputs pane. I want similar thing. I want it to be able to plot only the nets which are shown as "to be saved" in the outputs pane. I don't know why it's not working in my system even when using the same settings OR am I missing something else?

Please post the information we've asked for. We ask for it for a good reason, as it helps to understand what is going wrong. I am unaware of the simulating output information when it's been asked to only save a few nets - since you already said that the netlist was not the one you had a problem with, I'd sooner see the real data and then work backwards from that.

It's hard to know what you're missing if you don't show us what we've asked for...

I (re)started the simulation again yesterday itself with strobe period as 10n in transient analysis options to reduce the data. The simulation is going on currently. I'm not sure what I checked/unchecked in 'save device currents' line when the problem occured (first time simulation). But currently input.scs file is as follows:

Here you have chosen the signals to be output as "none". You really don't want that, because that will save only a single (arbitrarily chosen) signal - it was a historical limitation in spectre that it was hard to turn off the outputs completely, so "none" just picks one at random to get the results small.

Sir, even though it should save only 'vctl', I'm still able to plot other nets (Results -> Direct plot -> transient signal). Why is that so? (If it didn't save other nets, how is it able to plot them?) I hope you understood my doubt.

Could someone please reply to my doubt....Even though I want it to save only certain nets, spectre is saving every net clogging my hard disk. I cannot run a transistor level PLL with this problem.....please help.

Please note that Cadence AEs respond to questions on this forum often "off hours" and/or in addition to their "regular duties".

If this is a critical issue and you need immediate attention, please talk to your University staff and see how to file a Service Request at http://support.cadence.com . (There are specific instructions for university accounts).

I cannot reproduce what you are seeing in MMSIM 11.1 and IC 6.1.5 latest ISR.

If I only save one net. (save=selected) and

1. Select Results->Direct Plot->Transient Signal and click on an unsaved net, I get a message in the CIW:

*Warning* no "VT" data for node "/net8"

2. If I do not have any signal in the outputs pane selected for plotting, then I cannot use Results->Plot Outputs->Transient.

If I only have one signal selected in the Outputs pane, then I can only plot that signal.

3. Selct Results->Direct Plot->Main Form, I get an error in the Direct Plot form that says: